I'm more inclined to help somebody who includes a little profile info about himself and his background . . . but since you provided a link and attached the circuit file I'll give it a shot. (At least until I have to actually THINK about the problem - thinking makes my brain hurt.)

Computer programs like LTSpice are rather simple things. They tend to do EXACTLY what you tell them to do . . . which MAY (or may not) be what you want them to do. Your attached circuit file simulates nicely, and its simulated behavior agrees with my intuition for the topology and values you have entered. (I have not done any calculations to check against simulated results.)

Your big error is the capacitor values you specified. The original SPICE program expected capacitances to be specified in FARADS and LTSpice has adhered to this standard. Most practical capacitors have values in the MICRO-farad, or PICO-farad range. Consequently LTSpice sees your C1 as a 2,000 microfarad capacitor; C2 is 200 uFd. While probably not very realistic, these values are tolerable. The 200 uFd output coupling capacitor with the 8 ohm load should be flat to a few hundred Hertz if I remember correctly; this may not be your design goal but you can see it in an .ac analysis and easily correct it.

What is causing the simulation results to be different from your expectations is the compensation capacitor (C3) value. The web page for your circuit suggests that 500 PICO-farads is a suitable value. Your circuit file calls for 2000 MICRO-farads - a value FOUR MILLION times larger than shown on the web page!

LTSpice allows you to use letter abbreviations for many standard engineering power-of-ten notations. In this case, use the lower-case "u" in capacitor values to represent "micro-farads", and lower-case "p" for "pico-farads". (I think those letter abbreviations are accepted by default, but you might have to poke around in the "Control Panel" menu and check a box to activate that feature.) Other letter suffixes it recognizes include upper-case "K" for "kilo-", upper-case "G" for "gig-", and I think it accepts lower-case "n" for "nano-". BE CAREFUL with "M"!! That is used for "milli-", e.g. "10M" could be the value for a 10 milli-ohm current-sensing resistor. If you want to specify a 10 MEG-ohm resistor, you need to spell out "10MEG".

Once you have corrected that problem . . . the LED's you use in the bias networks are setting the idle currents way too high! I'll let you do a little background investigation to get a better understanding of why it works this way.

(You can use LTSpice to do some of this investigation. Look at the DC operating point voltages for the nodes associated with the bias networks, then compare them to the operating point voltages when you use the diode types specified on the web page where you found the circuit.)

The output transistors you chose (2N2222/2N2907) are really NOT suitable for driving an 8 ohm load. I'm not sure how the simulator will behave since you're asking it to operate these devices well outside their design envelope. (I don't know if the devices called for on your circuit's web page are available in a basic LTSpice installation or not. I've added quite a few devices to my "standard.bjt" file, so just because a device is listed on my installation doesn't mean it's available to you. You should learn how to paste device models right on your schematic diagram and call them out using the "Component Attributes" dialog but for the first few hours you play with LTSpice it's easier to use the built-in models.

While you're playing with this file . . . add some labels to a few of the nodes so you can easily refer to them by name rather than cryptic (and changeable) node numbers. Also consider changing a few of the component designators to more meaningful names.

See atch screen capture.

Dale

Noobert

25th April 2013 04:44 AM

Quote:

Originally Posted by dchisholm
(Post 3466267)

I'm more inclined to help somebody who includes a little profile info about himself and his background . . . but since you provided a link and attached the circuit file I'll give it a shot. (At least until I have to actually THINK about the problem - thinking makes my brain hurt.)

Computer programs like LTSpice are rather simple things. They tend to do EXACTLY what you tell them to do . . . which MAY (or may not) be what you want them to do. Your attached circuit file simulates nicely, and its simulated behavior agrees with my intuition for the topology and values you have entered. (I have not done any calculations to check against simulated results.)

Your big error is the capacitor values you specified. The original SPICE program expected capacitances to be specified in FARADS and LTSpice has adhered to this standard. Most practical capacitors have values in the MICRO-farad, or PICO-farad range. Consequently LTSpice sees your C1 as a 2,000 microfarad capacitor; C2 is 200 uFd. While probably not very realistic, these values are tolerable. The 200 uFd output coupling capacitor with the 8 ohm load should be flat to a few hundred Hertz if I remember correctly; this may not be your design goal but you can see it in an .ac analysis and easily correct it.

What is causing the simulation results to be different from your expectations is the compensation capacitor (C3) value. The web page for your circuit suggests that 500 PICO-farads is a suitable value. Your circuit file calls for 2000 MICRO-farads - a value FOUR MILLION times larger than shown on the web page!

LTSpice allows you to use letter abbreviations for many standard engineering power-of-ten notations. In this case, use the lower-case "u" in capacitor values to represent "micro-farads", and lower-case "p" for "pico-farads". (I think those letter abbreviations are accepted by default, but you might have to poke around in the "Control Panel" menu and check a box to activate that feature.) Other letter suffixes it recognizes include upper-case "K" for "kilo-", upper-case "G" for "gig-", and I think it accepts lower-case "n" for "nano-". BE CAREFUL with "M"!! That is used for "milli-", e.g. "10M" could be the value for a 10 milli-ohm current-sensing resistor. If you want to specify a 10 MEG-ohm resistor, you need to spell out "10MEG".

Once you have corrected that problem . . . the LED's you use in the bias networks are setting the idle currents way too high! I'll let you do a little background investigation to get a better understanding of why it works this way.

(You can use LTSpice to do some of this investigation. Look at the DC operating point voltages for the nodes associated with the bias networks, then compare them to the operating point voltages when you use the diode types specified on the web page where you found the circuit.)

The output transistors you chose (2N2222/2N2907) are really NOT suitable for driving an 8 ohm load. I'm not sure how the simulator will behave since you're asking it to operate these devices well outside their design envelope. (I don't know if the devices called for on your circuit's web page are available in a basic LTSpice installation or not. I've added quite a few devices to my "standard.bjt" file, so just because a device is listed on my installation doesn't mean it's available to you. You should learn how to paste device models right on your schematic diagram and call them out using the "Component Attributes" dialog but for the first few hours you play with LTSpice it's easier to use the built-in models.

While you're playing with this file . . . add some labels to a few of the nodes so you can easily refer to them by name rather than cryptic (and changeable) node numbers. Also consider changing a few of the component designators to more meaningful names.

See atch screen capture.

Dale

Thanks so much for your help. I made the changes you suggested. I changed the caps, the diodes (to those of the original circuit), voltage rails to 13.8v, added the models for the power transistors and the circuit seems to be amplifying properly.

I will be working on adding labels and learning exactly what each part/stage does tomorrow. Thanks again!

dchisholm

25th April 2013 09:42 PM

Quote:

Originally Posted by Noobert
(Post 3467472)

Thanks so much for your help. I made the changes you suggested. I changed the caps, the diodes (to those of the original circuit), voltage rails to 13.8v, added the models for the power transistors and the circuit seems to be amplifying properly.

I will be working on adding labels and learning exactly what each part/stage does tomorrow. Thanks again!

Your link gives an "Access not authorized" error.

You can often find simulation models by seeding a search engine with, e.g., "TIP41C SPICE". Another source is the "LTSpice" Yahoo group at http://tech.groups.yahoo.com/group/LTspice/ Please respect the members' time by searching the Files and old messages before posting "Can somebody send me a model for . . . ".

The quality and effectiveness of simulation models is a major topic by itself. The ones published by device manufacturers are usually OK for representing basic behavior in run-of-the-mill applications. You may also find some pretty crude models thrown together by individuals . . . . and in some situations a crude model is all you really need to investigate the behavior of a circuit. Occasionally you will find models that have been carefully crafted or modified by individuals to better represent some aspect of the physical component's behavior, or its behavior in certain situations. Bob Cordell's SPICE models are examples.

If you are studying this circuit as a way to learn about amplifiers (which is not a bad idea!), consider doing the following exercise, based on your observations from the circuit you first entered into LTSpice:

Learn to do a frequency response plot using the " .AC " analysis. Measure the upper and lower cutoff frequencies for your circuit.

Change some capacitor values, one at a time. The compensation capacitor might be a good place to start, since it's value was originally your most significant error. Increase, or decrease, its value by a factor of, say, 3 or 4. Then try a factor of 20 or 50. Or even 1000. What happens? Do you see why your original value gave the results you observed?

Do the same experiment with the input and output coupling capacitors. How do they affect overall performance?

Dale

Noobert

26th April 2013 03:44 PM

Quote:

Originally Posted by dchisholm
(Post 3468289)

Your link gives an "Access not authorized" error.

You can often find simulation models by seeding a search engine with, e.g., "TIP41C SPICE". Another source is the "LTSpice" Yahoo group at LTspice : LTspice/SwitcherCAD III Please respect the members' time by searching the Files and old messages before posting "Can somebody send me a model for . . . ".

The quality and effectiveness of simulation models is a major topic by itself. The ones published by device manufacturers are usually OK for representing basic behavior in run-of-the-mill applications. You may also find some pretty crude models thrown together by individuals . . . . and in some situations a crude model is all you really need to investigate the behavior of a circuit. Occasionally you will find models that have been carefully crafted or modified by individuals to better represent some aspect of the physical component's behavior, or its behavior in certain situations. Bob Cordell's SPICE models are examples.

If you are studying this circuit as a way to learn about amplifiers (which is not a bad idea!), consider doing the following exercise, based on your observations from the circuit you first entered into LTSpice:

Learn to do a frequency response plot using the " .AC " analysis. Measure the upper and lower cutoff frequencies for your circuit.

Change some capacitor values, one at a time. The compensation capacitor might be a good place to start, since it's value was originally your most significant error. Increase, or decrease, its value by a factor of, say, 3 or 4. Then try a factor of 20 or 50. Or even 1000. What happens? Do you see why your original value gave the results you observed?

Do the same experiment with the input and output coupling capacitors. How do they affect overall performance?

Dale

Thanks for your response.

I have already added the proper spice models to my spice directory. I was not asking for someone to find the models and do it for me. I was just stating that because I didn't want people to waste their time opening it if they couldn't simulate it without the models that I have. I suppose what I should have done is just posted the text here for each model that I added and others could add it to their libraries if they chose to view my circuit. Sorry for the confusion.

I am also sorry that I posted a link that was apparently not private. (wasn't thinking :( )

The circuit posted above still give me a very clean output with a gain of 10. I have changed some of the components to those that I have on hand so I could build it. I did build it and it does work, but sounds very bad. My goal is to make it sound good :).

My hope is to learn about amplifiers by studying this circuit. I appreciate the bullets you posted. I will be running through those exercises later today.

Thanks for your responses. I really appreciate your insight.

indianajo

26th April 2013 05:47 PM

Thanks for labeling your sample amp "compensation cap". I've repaired a few amps and read a lot of text here. I thought caps in that position (b-e on lower driver transistor) were just to prevent the output from radio frequency oscillating. The first transistor amp I repaired didn't have one from the factory; it was installed in a 3 year later modification. Will go back and read some threads and try to figure out what else designers are doing with it.
This is a simulation free zone unless I find a pspice program that is designed to work with Pentium IV CPU's with 500 MB ram and Linux op system. No money here for continual microsoft updates and upgrades. Easier and cheaper to build amps point to point on NEMA-LE boards and see what happens.

Noobert

28th April 2013 03:30 AM

Hello all, I finally got it working on my breadboard. It plays music, looks good on my scope (no noise/cutoff).

The only concern I have is that it has a gain of 8 and in simulation it had a gain of 10. What could have caused this? Thanks for your help.

JMFahey

28th April 2013 06:39 AM

Welcome to the real World ;)

Noobert

28th April 2013 02:44 PM

Quote:

Originally Posted by JMFahey
(Post 3470853)

Welcome to the real World ;)

:P. So I guess it's safe to assume, gain in a simulation isn't always the same as what is built in a real world circuit. Thanks.

Mooly

28th April 2013 02:54 PM

I would look a little harder at your built amplifier and compare the circuit and the passive component values to those used in the simulation.

The gain should be identical (to within minute limits) of sim vs actual build for a simple design like this . There will be a real reason why the two differ. It could be a component value error or even something like a wiring error where the feedback signal is getting "modulated" or modified due to "real world" wiring having resistance. Are you measuring the gain at "mid band" frequency where the capacitors reactive component is negligable ?